CamBam plus 0.9.8N (development release)

[rawkstar320]

way cool, Thanks Andy! Merry Christmas!

[pixelmaker]

Hello Andy,

many thanks for the new release and all the great updates. And I wish you a great new year.

With the rc7 I have some problems with the pp. I can´t get the toolchange to work.


ralf

[10bulls]

With the rc7 I have some problems with the pp. I can´t get the toolchange to work.

Oh no!
There were some changes relating to this.

Are you using the 'Tool Change' property from the Tool library, or are you using the {$tool.toolchange} macro in your post post processor?

[pixelmaker]

Hello Andy,

first I have to test something, befor I can describe it. But it looks that just the line "Tool Change" from the PP don´t work.
In this line I have:
{$clearance} {$tool.toolchange}
{$comment} T{$tool.index} : {$tool.diameter} {$endcomment}
T{$tool.index} M06

In 0.9.8N1 I get:
( Made using CamBam - http://www.cambam.co.uk )
( Ohne Namen 12/26/2012 3:25:52 PM )
( T1 : 1.0 )
( T2 : 2.0 )
( T3 : 3.0 )
G21 G90 G64 G40
G0 Z8.0
( TOOL/MILL,1.0,0.0,0.0,0 )
( COLOR,255,200,0 )
( T1 : 1.0 )
T1 M06
( Profil1 )
G17
M3 S18000
G0 X-25.0 Y-25.5
G0 Z1.0
G1 F300.0 Z-1.0
G1 F800.0 X25.0
G3 X25.5 Y-25.0 I0.0 J0.5
G1 F800.0 Y25.0
G3 X25.0 Y25.5 I-0.5 J0.0
G1 F800.0 X-25.0
G3 X-25.5 Y25.0 I0.0 J-0.5
G1 F800.0 Y-25.0
G3 X-25.0 Y-25.5 I0.5 J0.0
( Profil2 )
G0 Z8.0
( TOOL/MILL,2.0,0.0,0.0,0 )
( COLOR,150,255,0 )
( T2 : 2.0 )
T2 M06
M3 S18000
G1 F300.0 Y-26.0

In the N rc7 I get:

( Made using CamBam - http://www.cambam.co.uk )
( Ohne Namen 12/26/2012 3:30:30 PM )
( T1 : 1.0 )
( T2 : 2.0 )
( T3 : 3.0 )
G21 G90 G64 G40
( TOOL/MILL,1.0,0.0,0.0,0 )
( COLOR,255,200,0 )
G0 Z8.0
( Profil1 )
( TOOL/MILL,1.0,0.0,0.0,0 )
( COLOR,255,200,0 )
G17
M3 S18000
G0 X-25.0 Y-25.5
G0 Z1.0
G1 F300.0 Z-1.0
G1 F800.0 X25.0
G3 X25.5 Y-25.0 I0.0 J0.5
G1 F800.0 Y25.0
G3 X25.0 Y25.5 I-0.5 J0.0
G1 F800.0 X-25.0
G3 X-25.5 Y25.0 I0.0 J-0.5
G1 F800.0 Y-25.0
G3 X-25.0 Y-25.5 I0.5 J0.0
( Profil2 )
( TOOL/MILL,2.0,0.0,0.0,0 )
( COLOR,150,255,0 )
S18000
G1 F300.0 Y-26.0

All variables in the "Tool Change" are missed in the output.
Both versions of cambam are working with the same system folder, with exactly the same pp.
ralf

[10bulls]

{$clearance} {$tool.toolchange}
{$comment} T{$tool.index} : {$tool.diameter} {$endcomment}
T{$tool.index} M06

Can you try taking out the {$tool.toolchange} macro from the above?

This macro is no longer supported.
I am sorry about that, but the Tool - Tool Change behaviour was a bit mixed up previously.

It should now work so that if there is anything in the Tool - Tool Change property, it will override the post processor's Tool Change command.

If you just want to include something from the tool library (such as a custom tool definition for CutViewer) you can now add this in the Tool - Comment property, then in the post processor include it using {$tool.comment}

I hope this helps!

[dh42]

Hello 

I confirm that it works by moving the code from 'toolchange' to 'comment' in the tool library and replacing {$tool.toolchange} by {$tool.comment} in the pp.

++
David

[pixelmaker]

Hello Andy and David,
the problem was that also the {$clearence} don´t work.
What I try now is a fresh windows (no problem, only a 3gb file) with a fresh install of cambam rc7 and with the original default pp. There it works all ok.
But when I copy the original default pp into the old windows installation the same fault exists and all from the Tool Change line is missed.
Then it must be something going wrong with the update.

What I do now is to delete also this installation onto the old windows, reinstall the rc6 and do the update again.

ralf

[dh42]

Hello Ralf

Are you sure that the Toolchange property is empty on all the tools used ?

I see that even if just a single space or a non printable char remain in the Toolchange property and the PP don't write is default definition.

++
David

[pixelmaker]

hello David,

yes, that it was. After a lot of reinstalling, testing, copying every single file, I found it also.
After copying back my old tool library the error occurs.

It has nothing to do with the postprocessor, it is as you write. If any macro is in the Tool Change line of a tool in the library, the toolchange macro don´t work for this tool.


And I thought the problem are the 4 different installed versions of CamBam with only two system folders.
Now all is clean, I change all from the Tool Change Line to the Comment Line in the tools of my tool library and all works perfekt.

Thanks again Andy and David

ralf

[dh42]

It has nothing to do with the postprocessor, it is as you write. If any macro is in the Tool Change line of a tool in the library, the toolchange macro don´t work for this tool.

Yes in the new version, a macro in the tool.toolchange property replace all the definitions in the pp by the definition in the tool.toolchange.

3 way:

1- add the {$clearance} and  T{$tool.index} M6 in the definition of the macro of each tool (in addition to your custom macro).

2 - use the new {$post.toolchange} macro in you tool definition ; this macro return the definition that is in the pp, and you can of course add additional code.

3 - if it's just to add some CutViewer definitions, use only the new tool.comment property for the CV defs and let the tool.toolchange property blank. In this case you must use the macro {$tool.comment} in your pp to add this comments (and remove the {$tool.toolchange} that no longer exists.

++
David

[pixelmaker]

I use now in the line Tool Change of the pp:
{$clearance}{$tool.comment}
{$comment} T{$tool.index} : {$tool.diameter} {$endcomment}
T{$tool.index} M6

The {$toolchange} in the pp is still the same and I have it for every tool. In the tools I use now only the comment line for the CV comments.

I think for a normal user who works with CutViewer it is more simple to change {$tool.toolchange} into {$tool.comment} in the Tool Change Line of the pp and in the tool library cut and paste the macro line with cutviewer comments into the new comment line in every tool.
And the result is the same. I don´t know why to add the "{$clearance} and  T{$tool.index} M6"  to every tool.

If a macro in the tool.toolchange property overrides properly the toolchange property in the postprocessor (I am happy that I can write this and must not speek this)  then a {$clearence} in this line must arrive in the g-code, but this isn´t.

In the tools new Comment property I use for CV:
{$comment} TOOL/MILL,{$tool.diameter},{$tool.radius},{$tool.length},0 {$endcomment}
{$comment} COLOR,44,190,6 {$endcomment}

ralf

[10bulls]

Development release 0.9.8N (rc-8) is now available for download...

http://www.cambam.info/downloads/#devt

In this release...

* The occasional property grid lock-up bug should be fixed.
* Some more changes regarding 3D surface boundaries.
The 'Unhandled error' with bounding box boundaries and some others should be fixed.
The boundaries can now support 'Region' shapes when selected shape boundaries are used...so you could restrict machining to a torus shape for example.
* {$xneg} {$yneg} {$zneg} {$ineg} {$jneg} {$xabs} {$yabs} {$zabs} {$iabs} {$jabs} post processor macros are working again now.
There were also a couple of changes made so the above macros could be used to set up a post processor for machines that have Y and Z inverted.
* Lathe diameter mode with arc polylines (usually in finishing) bug fixed.
* Toolpath optimisation bug with 'hatch fill' pockets fixed.
http://www.cambam.co.uk/forum/index.php?topic=3032.0
* Fixed bug with CamBam restoring to a tiny window if CamBam is closed when minimized.
* The NCFile machine operation 'Source File' property has been modified to support relative paths.
A g-code filename with no path is assumed to be in the same folder as the parent CamBam file.
This should allow CamBam files with ncfile operations to be more portable.
* Toolpath to geometry should now work with holding tab toolpaths now.

Thank you everyone for all your bug reports and feature requests!

[dh42]

Hello Andy,

Thanks for this release 

++
David

[Bubba]

Thank you, Andy.

[Dragonfly]

Default PP in the options seems to be a new thing.
Thanks.